CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ANSYS Meshing] 2D hexa mesh

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   July 4, 2013, 11:01
Default 2D hexa mesh
  #1
MVS
New Member
 
Marie
Join Date: Jul 2013
Posts: 3
Rep Power: 4
MVS is on a distinguished road
Dear all,

I am currently trying to mesh a very simple geometry in 2D that consists in a rectangular enclosure full of water and a PMMA plate near one of the walls.
I am more used to ICEM for meshing geometries like this, but I am currently working with ANSYS Workbench (v12), so the mesher is ANSYS Meshing.
I would like to know if it's possible with this mesher to do the same kind of mesh as with the "Blocking" method in ICEM ?
At first I used the Sweep method, but some tetra were generated and they seem to affect my solution (local high velocity divergence where the mesh is not pure hexa... )
Actually I already read about the Multi-zone mesh type but it does not let me put the inflation correctly on every wall...
I have also read the Meshing Help but I could not find any way to specify for instance the number of division along an edge or the growth ratio (as it could be found in ICEM).

Do you have any suggestion please ? I would be really grateful...
Thank you
MVS is offline   Reply With Quote

Old   July 4, 2013, 11:38
Default
  #2
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,098
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
There are some of the ICEM functionalities implemented in the latest versions of the Ansys mesher, but I dont think v12 already has it.

You can still get fairly good control over the mesh by splitting your geometry into smaller parts with 4 edges each (just the way you would do a blocking in ICEM).
Alternatively, if you are creating the geometry in Design modeler, dont create the whole geometry at once but the individual "blocks" of the geometry.
Just remember to "freeze" the parts before splitting them. Afterwards, you should select all the small parts together, right-click and "form new part".

Now in the Ansys mesher, you apply a "mapped face meshing" to all the faces.
Now with the "edge sizing" option, you can explicitly control the number of "cells" in each "block". Just remember to switch off the "use advanced size function" of the mesh and setting the "behavior" of the edge sizings to "hard".

Pretty easy, isnt it?
flotus1 is offline   Reply With Quote

Old   July 4, 2013, 11:45
Default
  #3
MVS
New Member
 
Marie
Join Date: Jul 2013
Posts: 3
Rep Power: 4
MVS is on a distinguished road
Thank you very much for your quick answer.
I already tried creating several "blocks" in Design modeler (as I would do in ICEM), sorry for not specifying this on my first post. However, There are some steps I might not have done correctly, I will check with what you just said.
Thank you so much again.
MVS is offline   Reply With Quote

Old   July 5, 2013, 04:19
Default
  #4
MVS
New Member
 
Marie
Join Date: Jul 2013
Posts: 3
Rep Power: 4
MVS is on a distinguished road
Hi flotus1,

I just wanted to thank you again: thanks to your advice, I could successfully generate the mesh I wanted (I used the spheres of influence because otherwise I could not get the inflation I wanted).
However the last time I tried creating the geometry by splitting it into "blocks", I had high velocity divergence at the fluid/fluid interfaces... Maybe the new mesh will solve this problem (I hope so).

Thank you again for you help !
MVS is offline   Reply With Quote

Old   July 5, 2013, 06:16
Default
  #5
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,098
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
If you apply the "form new part" option in design modeler to create ONE part containing all the "blocks", there should not be any fluid-fluid interfaces at all.
flotus1 is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
3D Hybrid Mesh Errors DarrenC ANSYS Meshing & Geometry 11 August 5, 2013 06:42
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation tommymoose ANSYS Meshing & Geometry 48 April 15, 2013 04:24
[ICEM] export hexa mesh to fluent Wieland ANSYS Meshing & Geometry 37 January 23, 2013 04:27
[ICEM] Hexa Mesh Smoothing Jules ANSYS Meshing & Geometry 6 December 4, 2010 19:00


All times are GMT -4. The time now is 14:00.